Use Alibre's New 3D Sketch to Quickly Modify Complex Shapes

The new 3D Sketch capability in Alibre Design v8 lets you create freeform 3D curves and lines that can be used in modeling operations to define sweep paths for piping applications and guide curves for lofting operations. Plus, 3D sketches can be associated to 2D sketches and solid bodies to create guide curves for better control of lofts. This month's column will show you how to build a sample model using associated 2D sketches and 3D guide curves.

Creating Complex Shapes with 3D Sketch and Loft
Begin the process by making sure Snap to Working Plane is checked in the Tools / Options dialog box. This option is on the General tab under Design. To start the model, first create three 2D sketches to serve as cross-sections. To create the first cross-section (figure 1):

In the Work Area, right-click the XY Plane and choose Activate 2D Sketch.

Select the Circle tool and create a circle with the center point at the origin.

To set the size of the circle, select the Dimension tool and click the circle. Click again to place the dimension and enter 3.0 in the dialog box.

Exit Sketch mode by clicking the 2D Sketch tool.

Figure 1. This circle will act as the first cross-section.

Now create the second cross-section (figure 2):

Select View / Orientations, then double-click Isometric.

In the Design Explorer, right-click the XY Plane and choose Insert Plane. Set the Plane Offset Distance to 5.0. Check the Reverse option, then select OK. You may need to zoom out to see the new plane.

Note: You can insert a negative value instead of using the Reverse option.

Figure 2. Create a new plane for the second profile.

Now add dimensions to the ellipse (figure 3):

In the Work Area, right-click the new plane and select Activate 2D Sketch.

From the Sketch menu, select Figures / Ellipse.

Click the origin to set the center of the ellipse. Drag the mouse upward and click to set the major radius. Drag outward and click to set the minor radius.

Click the Dimension tool, then select the center node and the node on the top of the ellipse. Set the dimension to 1.25.

Also using the Dimension tool, select the center node and the node on the side of the ellipse. Set the dimension to 0.75.

Exit Sketch mode.

Figure 3. Apply dimensions to the ellipse figure so it is smaller than the circle figure.

From the Sketch menu, select Figures / Rectangle / Two Corners. Click in the upper left area within the circle as shown to set the first corner, then click in the lower right area within the circle.

Apply a constraint to make the sides equal, then use the Dimension tool to set the length of one side to 2.0.

Also using the Dimension tool, click the origin and one side, then set the dimension to 1.0. Repeat to set the distance from the origin to the top side to 1.0.

Exit Sketch mode.

Figure 4. Apply dimensions to the square figure.

Take a look at the sketches in 3D space (figure 5). To rotate the model, press both mouse buttons and move the cursor. Release when the desired orientation is achieved.

Figure 5. The three sketches will be used as profiles for the final part.

To hide the Planes, select View / References / Planes if it is checked. From the Tools menu, select Options and click the Grid tab. Uncheck the Snap to Grid option. This will make it easier to place and move nodes on the 3D spline.
Now create the 3D spline (figure 6):

Select Activate 3D Sketch from the 3D Sketch menu.

Select the Spline tool. To create a curve that passes through the three cross-sections as shown below, click the first two sketches once and double-click the last to complete the spline.

Figure 6. A 3D guide curve associated with sketches 1, 2 and 3.

For additional control, you can insert and freely position more spline nodes (figure 7).

Select the Insert Node Into Spline tool from the fly-out toolbar under the Spline tool. Click the spline approximately midway between the existing nodes to insert two additional interpolation points.

To reposition the nodes, click the Select tool from the Sketch toolbar and drag each node.

Note: Cursor movement is controlled by the active sketch plane. The spline node will only move in directions parallel to the sketch plane. To move the node in another direction, use the F key to cycle to a different plane. Also, you may add dimensions to the Spline to precisely define the shape at any time during geometry creation.

Figure 7. Adjust the guide curve for more control over the shape of the part.

About the Author: Michael Todd

In her easy-to-follow, friendly style, long-time Cadalyst contributing editor and Autodesk Technical Evangelist Lynn Allen guides you through a new feature or time-saving trick in every episode of her popular AutoCAD video tips. Subscribe to the free Cadalyst Video Picks newsletter and we'll notify you every time a new video tip is published. All exclusively from Cadalyst!